Comparison of OF and Fluent results
 

Hi everyone!
I want to move from calculations in Fluent to the OF. To do this, we compared the results obtained in both programs.

Problem: turbulent flow in a circular channel.
Fluent boundary conditions:
k-w SST turbulence model;
SIMPLE solver scheme;
Inlet velocity 10 m/s;
Turbulence intensity at inlet and outlet 4%;
Pressure outlet 0 Pa.
Geometry:
Circular cross-section channel,diameter 0.1 m, length 100D.
Symmetry on XY, ZX.

The mesh was created in Ansis meshing and transferred to OF via "Fluent3DMeshToFoam"
The first case of the mesh with y+=1 was with the warning "Failed 1 Mesh Checks" and the calculations did not coincide.
The second case with a mesh with y+=94 completely coincided with Fluent.
Attachment 87406
Attachment 87411
Attachment 87412

OpenFoam bc:
Attachment 87407
k, w, vel, nut same to Fluent.

Please tell me where the error is or why the rough mesh matches the results. What boundary conditions should be set for the mesh with y+=1.

continuation
 

Obtained data
Attachment 87414
Attachment 87415
Attachment 87416
Attachment 87418
Attachment 87419

The mesh check is telling you that the max cell aspect ratio is too high (1922) for your y+=1 mesh ... this can screw up the gradient calculations, since the wall normal gradient component of a variable is so much larger than the streamwise gradient component simply due to the cell dimensions. This means that the solution can decouple, which is maybe what you are seeing.

You can try using something like the leastSquares gradScheme approach which helps counter this, but in reality the best solution is, as ever, to just improve your mesh. If you want to minimise your cell count then just grab the near wall cells that have aspect ratios above 100 and use refineMesh to refine them in the axial direction; you'll need several nested refinements to get the near wall cell ARs down to around 100. That should then help.

Good luck!